Dear all
I want to change different material properties(Young's Modulus and Poisson's Ratio) of all the mesh elements of a solid block having 50000 finite elements in ANSYS APDL. I have the values of Young's Modulus and Poisson's Ratio for each element in an array but I don't know how to update the values for such a huge number of elements.
Any help regarding this is highly appreciated.
Thank You in Advance.
i feel you need divide the mesh into number of regions, if you want to change the material properties for each regions..you double click on individual regions that you divided now assign the material properties for each regions. i hope this approach may work in your case..ok all the best..
Dear Prof. Karthigeyan . S thanks for your suggestion.The problem is I need to update the material property after each and every iteration and changing the mesh into number of regions every time might be cumbersome.
Actually I have tried with lesser number of elements with ESEL followed by MPCHG command and it worked fine but in that case I have manually selected number of elements say from elem no. 1 to 10 and changed the material properties for those elements. But I don't know how to proceed when the number of elements are huge and manual picking is cumbersome.
Rajdeep Ghosh can you help me regarding updating the material properties as per the stress in the element in ansys?
@ Rajdeep ghosh can you help me with regarding updating the material properties for each and every element in ANSYS APDL?
Minku Arora As rightly mentioned by Dr Bendine, first select those elements you want to modify using ESEL and then you can use the *DO loop for all those selected elements followed by the EMODIF command. For details about those commands, you can check ANSYS APDL command references easily available on the internet.
*DO loop actually automates the EMODIF process for all those selected elements and thus helps you by saving your valuable time if you want to run your FE model iteratively. Otherwise, you can also manually select elements of a particular element type you want to modify and then use the EMODIF command.
Best Wishes
Thanks you for your response.
But i have a text file which contains different material property for each and every element. How to assign this property to each and every element?
*do,i,1,MAXELE,1
EMODIF, i , MAT , i
*enddo
This will assign the material number to each element. But how to first assign the properties with MP for each element?
Minku Arora
u can use the following code as a guide for your problem
!Read material property txt data
*DIM,XG,TABLE,MAXELE,1,0, , ,
*TREAD,Em,'MatProp','txt',' ', ,
*Do,i,1,MAXELE,1
ESEL,S,cent,X,i ! Select the element number
MP, ex, i, Em(I,1) ! Assign the corresponding youngs modulus
EMODIF, i , MAT , i
*Enddo
Dear Kouider Bendine ,
Suppose we now have MAXELE elements with only 4 distinct material types, already defined in APDL. A txt file of MAXELE lines containing one integer per line (i.e. 1, 2, 1, 1, 3, 4, ..., 1) associates each element to each material type. How would you do use this in APDL, please? I have tried the following, unsuccessfully:
*DIM,MATVALS,ARRAY,MAXELE,1
*VREAD,MATVALS(1),'mat_vals','txt'
(I) ! specifies integer format
*DO,I,1,MAXELE,1
EMODIF, I, MAT, MATVALS(I)
*ENDDO
It seems that ANSYS does not iteratively access the array MATVALS(I)
I've figured out my problem. It seems that you have to specify the array as a float, instead of an integer.
Therefore, all of the values in mat_vals.txt in my example have to be floats, e.g. 1., 2., 1., 1., 3., 4., ..., 1.. And then the working example becomes:
*DIM,MATVALS,ARRAY,MAXELE,1
*VREAD,MATVALS(1),'mat_vals','txt'
(F) ! specifies float format
*DO,I,1,MAXELE,1
EMODIF, I, MAT, MATVALS(I)
*ENDDO
Or, even faster, using implicit looping:
*DIM,MATVALS,ARRAY,MAXELE,1
*VREAD,MATVALS(1),'mat_vals','txt'
(F)
EMODIF, 1:MAXELE, MAT, MATVALS(1:MAXELE)
- Badges
- Science topic
- Similar topics
- Engineering
- Mechanical Engineering